Machine and Tool Offsets

Fixture Offset XY

Figure 5.2 shows a plan view of how the Fixture Offset XY works. The CNC operator finds the fixture offset values by jogging (moving) the machine from the machine at its home position the CNC program datum. This can be any point on the part, stock, or fixture, as long as it can be found by mechanical means such as an edge finder or part probe.

The incremental X and Y distances moved between points is recorded and entered into a Fixture Offset Register on the CNC control. Think of the Offset registers like a table in a spreadsheet. The CNC control references these values in the table each time a motion is commanded, adding or subtracting them from coordinates in the CNC program. In other words, Fixture XY offsets convert Machine Coordinates into WCS coordinates.

Most machine controls support at least six fixture offsets, labeled G54 thru G59. Multiple registers are needed because most parts use a different fixture offset for each side of the part machined.

Figure 5.2: Fixture Offset Plan View

The Fixture Offset Z-coordinate is not used to shift the Machine Z. Use of the Fixture Offset Z is covered in the next topic.

Fixture Offset Z

The purpose of the Fixture Offset Z is to record the incremental distance from a tool setting position to the part datum. The tool set position can be a tool probe or, as shown in Figure 5.3, the top of a precision 1-2-3 block set on the machine table. The approach shown in Figure 5.3 involves using a dial indicator and this process is detailed in Set Fixture Offset Z.

The CNC control adds the Fixture Offset Z and Tool Length Offset for the active tool together to calculate the distance from the tip of each tool at Home to the Z-datum on the part.

Figure 5.3: Fixture Offset Z

There are many ways to set tool and fixture offsets. The method described here and detailed in Set Fixture Offset Z, is precise, compatible with tool probe systems, and easy to understand and use once tried just a few times. Another advantage is that the TLO can be reset easily, even if the part datum has been machined away, which is common with 3D parts.

Appx B - Alternate Tool Setting Methods describes three other methods that can be used to set up the machine tool length offsets.

To use the method described in this chapter on Haas Automation machines, machine control parameter 64 (T OFS USES WORK) must be set to OFF. Refer to the Haas Programming and Operation manual for instructions on set this parameter.

Tool Length Offset (TLO)

Every tool loaded into the machine is a different length. In fact, if a tool is replaced due to wear or breaking, the length of its replacement will likely change because it is almost impossible to set a new tool in the holder in exactly the same place as the old one. The CNC machine needs some way of knowing how far each tool extends from the spindle to the tip. This is accomplished using a Tool Length Offset (TLO).

The TLO is found by jogging the spindle with tool from the machine home Z-position to the tool setting point on the machine. This can be the top of a tool probe, or as shown in Figure 5.4, the top of a 1-2-3 block resting on the machine table. The distance travelled from home to the top of the block is recorded, and the value entered into the TLO register for that tool (called an H-register, because it is preceded by the letter H in the CNC program).

If a tool wears or breaks, it can be replaced, the H-register reset to the new tool by touching off again on the 1-2-3 block, and the program continued with no other changes.

Figure 5.4: Tool Length Offset